some beginners questions 3

[HonzaS]

Hi,

1) Could I move the end of section line farther away the view? It wasn`t problem in Inventor, but I don`t know how to do it in NX. (attached picture 01)

http://files.engineering.com/getfile.aspx?folder=158b9998-373b-45a5-8c55-b9e5b75f7ccb&file=01.JPG

2) Is it possible to delete a line from drawing?

3) How to align these dimension? Each of them wants to be in the middle of its arrow line. Or how to swich off its snapping?

(

http://files.engineering.com/getfile.aspx?folder=39436f3f-381e-4a98-9a58-87de7547a6fd&file=04.JPG)

4) In modelling: Does exist some function to substructing body by swept? I can use for example swept sheet, then trim body, then trim sheet, but it is quite strange. ))

(

http://files.engineering.com/getfile.aspx?folder=14a398e9-ce2a-43cf-a8a8-96bf29b3c156&file=03.JPG)

Thanks a lot

 

[MickyV007]

1) RM click on the arrow, choose Edit... then in this menu choose Move Segment, click on the arrow and click on the drawing sheet at the disered place where you want your arrow.

2) 2 ways, first RM click on a view, choose View Dependent Edit, in the Add Edits choose the first option (Erase Objects) click the lines you want to delete, push OK.

3) Goto Preferences menu, Annotation, in this menu goto first tab - Dimensions, right beneath this tab is a pull down menu choose Automatic Placement.
Or double click on the dimension (now you see the Edit Dimension toolbar), then RM click on that same dimension, there is a Placement tab, choose Automatic dimension here.
Or in the Edit Dimension toolbar choose Style, you get a new menu where you can choose Automatic Placement.

4) As for this question, i think you need to create a solid instead of just one curve to creat this substract with a swept (but i'm not 100% sure)

Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native

 

[HonzaS]

MickyV007
1),2) works .. thanks

3) I have tried the each combination of those three buttons. But when I moved with the lettering around the middle of arrow line, it ever jumped exactly to the middle.
So when I would like to have these lettering aligned, I have to put them near one of arrows.

(

http://files.engineering.com/getfile.aspx?folder=ac84623d-4703-45d5-89df-acf9e78be92a&file=05.JPG)

4) I can create the solid body by function swept, but there isn`t the choice of boolean type - subtract.

 

[MickyV007]

3) you choose Automatic Placement as you want your dimension in the center of the line, you can also use Manual placement (arrows in and arrows out) to place the dimension on a random place.
Maybey you are struggling with the snap from one dimension to another? You can switch off this behaviour by holding down the ALT key when you are moving a dimension, give it a try.

4) No there is no build in Boolean operation like Substract in the Swept menu.

Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native

 

[HonzaS]

3) Alt key - that`s what I was looking for.

4) Does anybody know some alternative function?

 

[cowski]

4) sweep it and then perform a subtract OR sweep a sheet and trim the solid body - a perfectly valid operation.

 

[cowski]

I can use for example swept sheet, then trim body, then trim sheet, but it is quite strange. ))

Why do you trim the sheet after you trim the body?

 

[HonzaS]

cowski:
I didn`t try Sweep along guide. It works. There is a subtract choice..

But Swept has better options as regards a section orientation.
So I create a sheet and trim a body. But then I don`t know how to get rid of the sheet.
That`s the reason why I trimmed the sheet. Anyway the sheet still stay on the new body section..

 

[cowski]

You can hide the sheet (edit -> show and hide) or place it on a different layer (then make the layer invisible).

 

[HonzaS]

Hidden feature is still on the drawing. I have to move it into a invisible layer. I have never used it. Thanks

 

[JohnRBaker]

You can also go back to the original part and edit the Model Reference Set by going to ...

Format -> Reference Sets...

...and selecting the 'Model' Reference Set in the list and deseletcing the Sheet Body(s) which will remove them from the Reference Set and thus from the Drawing as well.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

This assumes you are using the master model approach (drawing and model in separate files). If you keep the drawing in the same file as the model (possible but not recommended) you will probably have to use layers.

 

[JohnRBaker]

If he's a 'beginner' let's hope he's using the Master Model approach as we do NOT want anyone to pick up any bad habits this early, now do we ;-)

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

Yes, I hope they are using master model, but there is nothing in the post to prove that one way or the other. If he isn't using master model, steering him toward reference sets could be quite confusing.

So, for the record the best practice is: use the master model approach and use reference sets for the geometry you want in the assembly and/or drawing.

 

[HonzaS]

Interesting.
It can be done everything. Just to know how =))

 

[JacqSkylark]

Hi All
This is my first post.
How to make the radial menu in NX 7.5? shift+ctrl+LPM; shift+ctrl+SPM i shift+ctrl+PMP I known but I'm interesting about view like in Solid Edge ST3.
Thanks

 

[HonzaS]

Just one question:
5) How to fix surface finish symbol to a line in drawing. It works only when there is a leader otherwise the symbol stays on the same place after moving a view.
I tried to set associativity to the view, but the symbol became smaller..?

Thanks